[Ho_Sh]

Hello,

I am simulating a heat exchanger based on the TPMS core. I created the geometry on nTopology platform and transferred it to CFX for simulation. But CFX cannot distinguish between the interfaces, so I had to delete the solid which left a gap between hot and cold fluid. When I run the simulation in this way, no heat transfer occurs, although it converges.

I use the mass flow rate and temperature of inlets to find the outlet temperatures and pressures.

Any idea if there is any way to overcome the issue?

Many thanks
Hossein

[ghorrocks]

Umm, isn't it obvious? You need to put the solid back in and sort the interfaces out.

Different meshing packages have different approaches to meshing multiple bodies and labelling the resulting mesh. You need to figure out a way of doing this which works with your mesher.

Note the default interface generator in CFX-Pre can give poor results in some cases, so you sometimes need to turn it off and assign the interface faces yourself. This is where the mesher is important - if you have labelled the faces carefully then they should be available in the CFX-Pre region selection box. If not, then you have to manually select all the surfaces. Manually selecting them is OK for models which are not too complex (I have done this many times).

[Ho_Sh]

Thanks, Glenn. Sorry for getting back so late. Can I ask what you mean by labelling the faces carefully? I use nTopology software to create the geometry and the mesh. When I transfer the meshed file to CFX, I get the message which says the surface has already been used, which correlates with what you said above. But my geometry is very complex, and literally impossible to assign the interface manually.

So I decided to remove the solid and run the simulation with the gap between cold and hot fluid and use the Face Intersection Depth Factor to run it. The problem is the heat transfer is not happening.

Can I ask if heat transfer simulation through the gap is doable on CFX? If so, what can I do to make it work?

Thank you, and I apologise again for the late response.

Hossein

[Gert-Jan]

You should:
- remove the thin solid from your geometry
- create 2 fluid volumes on both sides with unique names.
- extrude the faces to touch each other where the thin solid was. This will be your interface
- mesh the volumes with a conformal mesh on the interface
- Import the mesh in CFD-Pre. If everything went alright, CFX-Pre will put both volumes in a single Default Domain.
- Where your solid was, create an interface
- You can assign properties to this interface as if it is a solid with a certain thickness and conductivity.

[Ho_Sh]

Thank you for the detailed solution. I will try that to see how it works. Regards.